rhoSimpleFoam unknown RASModel type laminar

tdog · June 6, 2016, 10:40

Hello
I'm trying to do a compressible simulation using rhoSimpleFoam for a laminar flow. The scripts I am using is based on an earlier OpenFOAM version (2.0 I think) as was working there, but I am running the newest version.

When I run my scripts I get the following error:
"--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
"
Where my turbulenceProperties is set to the following:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  RAS;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //

As far as I can tell from the documentation (http://cfd.direct/openfoam/user-guide/turbulence/) I am doing it the right wa, what seems to be the problem?

tdog · June 7, 2016, 16:40

Has nobody tried something similar?

vabishek · June 8, 2016, 09:38

Quote:

Originally Posted by tdog

Hello
I'm trying to do a compressible simulation using rhoSimpleFoam for a laminar flow. The scripts I am using is based on an earlier OpenFOAM version (2.0 I think) as was working there, but I am running the newest version.

When I run my scripts I get the following error:
"--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)
"
Where my turbulenceProperties is set to the following:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  RAS;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //

As far as I can tell from the documentation (http://cfd.direct/openfoam/user-guide/turbulence/) I am doing it the right wa, what seems to be the problem?

Not sure if you have fixed it yet but the simulationType should be set to "laminar". If you read the above documentation carefully, it is mentioned at the very beginning.

tdog · June 8, 2016, 10:20

@vabishek thank you for your help. I already tried that, but it still produces the same error:
Selecting RAS turbulence model laminar

--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  laminar;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //

vabishek · June 8, 2016, 10:24

Quote:

Originally Posted by tdog

@vabishek thank you for your help. I already tried that, but it still produces the same error:
Selecting RAS turbulence model laminar

--> FOAM FATAL ERROR:
Unknown RASModel type laminar

Valid RASModel types:

12
(
LRR
LaunderSharmaKE
RNGkEpsilon
SSG
SpalartAllmaras
buoyantKEpsilon
kEpsilon
kOmega
kOmegaSST
kOmegaSSTSAS
realizableKE
v2f
)

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v3.0+                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType  laminar;

RAS
{
    RASModel        laminar;

    turbulence      off;

    printCoeffs     off;
}


// ************************************************************************* //

Well, it should look something like this

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

simulationType laminar;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}


// ************************************************************************* //

As the error message says, just pick one RASModel from the given list. As you can see, "laminar" is not listed there. If you set simulationType to laminar, it doesn't really mattter what you set RASModel to. Hope that helps!

tdog · June 8, 2016, 10:54

Arg, thanks for the tip

Just tried, but still got an error message because I then need to supply files for the boundary conditions - because in theory it shouldn't need them because it's running the simulation as laminar, but those are turbulent models, right?

pupo · June 9, 2016, 07:32

This bug seems to have been fixed "recentely"

check the following Commit: https://github.com/OpenFOAM/OpenFOAM...2940548af3ebb3

If your createFields.H in BuyoantSimpleFoam looks like this:

Code:

autoPtr<compressible::RASModel> turbulence
(
     compressible::New<compressible::RASModel>
      (
          rho,
          U,
          phi,
          thermo
     )
 );

change it to:

Code:

autoPtr<compressible::turbulenceModel> turbulence
 (
     compressible::turbulenceModel::New
      (
          rho,
          U,
          phi,
          thermo
     )
 );

cheers

peterf · June 11, 2016, 06:31

I can't locate the applications folder in order to change createFields.H. How do I do this?

I am running OpenFOAM via Docker on a Mac. So I don't really see a path or folder for OpenFOAM. I have tried to show the hidden folders, but the OpenFOAM or applications folder still doesn't appear.

cleoo · September 9, 2016, 04:58

Quote:

Originally Posted by vabishek

Well, it should look something like this

Code:

simulationType laminar;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}

does it actually read the entries in the RAS part if you specified the simulationType as being laminar?

whats the difference between this:

Code:

simulationType RAS;

RAS
{
    RASModel        kOmega;

    turbulence      off;

    printCoeffs     on;
}

and

Code:

simulationType laminar;

because isn't turbulence off technically just laminar flow?

June 6, 2016, 10:40	rhoSimpleFoam unknown RASModel type laminar	#1
tdog New Member Thomas A Join Date: Mar 2016 Posts: 18 Rep Power: 10	Hello I'm trying to do a compressible simulation using rhoSimpleFoam for a laminar flow. The scripts I am using is based on an earlier OpenFOAM version (2.0 I think) as was working there, but I am running the newest version. When I run my scripts I get the following error: "--> FOAM FATAL ERROR: Unknown RASModel type laminar Valid RASModel types: 12 ( LRR LaunderSharmaKE RNGkEpsilon SSG SpalartAllmaras buoyantKEpsilon kEpsilon kOmega kOmegaSST kOmegaSSTSAS realizableKE v2f ) " Where my turbulenceProperties is set to the following: Code: /--------------------------------- C++ -----------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: v3.0+ \| \| \\ / A nd \| Web: www.OpenFOAM.com \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object turbulenceProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // simulationType RAS; RAS { RASModel laminar; turbulence off; printCoeffs off; } // ************************************************************************* // As far as I can tell from the documentation (http://cfd.direct/openfoam/user-guide/turbulence/) I am doing it the right wa, what seems to be the problem?

June 9, 2016, 07:32		#7
pupo Member Pedro Join Date: Nov 2014 Posts: 50 Rep Power: 11	This bug seems to have been fixed "recentely" check the following Commit: https://github.com/OpenFOAM/OpenFOAM...2940548af3ebb3 If your createFields.H in BuyoantSimpleFoam looks like this: Code: autoPtr<compressible::RASModel> turbulence ( compressible::New<compressible::RASModel> ( rho, U, phi, thermo ) ); change it to: Code: autoPtr<compressible::turbulenceModel> turbulence ( compressible::turbulenceModel::New ( rho, U, phi, thermo ) ); cheers

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Commercial meshers] Mesh conversion problem (fluent3DMeshToFoam)	Aadhavan	OpenFOAM Meshing & Mesh Conversion	2	March 8, 2018 01:47
time step continuity problem in VAWT simulation	lpz_michele	OpenFOAM Running, Solving & CFD	5	February 22, 2018 19:50
Divergent with rhoSimpleFoam and the boundary condition problems	qjh888	OpenFOAM Running, Solving & CFD	0	May 17, 2016 20:31
Boundary Conditions	MtnRunBeachBum	OpenFOAM Pre-Processing	1	April 30, 2015 16:33
compressible two phase flow in CFX4.4	youngan	CFX	0	July 1, 2003 23:32

June 7, 2016, 16:40		#2
tdog New Member Thomas A Join Date: Mar 2016 Posts: 18 Rep Power: 10	Has nobody tried something similar?

June 8, 2016, 10:54		#6
tdog New Member Thomas A Join Date: Mar 2016 Posts: 18 Rep Power: 10	Arg, thanks for the tip Just tried, but still got an error message because I then need to supply files for the boundary conditions - because in theory it shouldn't need them because it's running the simulation as laminar, but those are turbulent models, right?

June 11, 2016, 06:31		#8
peterf New Member Peter F Join Date: Jun 2016 Posts: 1 Rep Power: 0	I can't locate the applications folder in order to change createFields.H. How do I do this? I am running OpenFOAM via Docker on a Mac. So I don't really see a path or folder for OpenFOAM. I have tried to show the hidden folders, but the OpenFOAM or applications folder still doesn't appear.